If this is your first visit, be sure to
check out the FAQ by clicking the
link above. You may have to register
before you can post: click the register link above to proceed. To start viewing messages,
select the forum that you want to visit from the selection below.

Laser vector offsets (g-code?)...

I have an Epilog Zing-24, and have recently started using it to cut acrylic parts for prototyping. Usually, I take a SolidWorks drawing, create a drawing, export it as a DXF file, pull it into Corel Draw, and then I have to go into the drawing, and draw offsets to each line I want to cut, to make up for the beam width, or the final parts come out either too small or too large. Re-drawing everything using offsets, is painful and time consuming. I cannot just go into solidworks and make everything bigger or smaller, because later on, if I want to cut the same part on CNC mill, I will have trouble there.

Does anyone have any easy solution to this problem?

Normally, on any other CNC machine, I would pull the part into a CAM package, specify the toolpath, and the size of the tool is automatically handled by the CAM package. Perhaps there is a way to control the Zing with some g-code? Then I could use a CAM package to generate the laser path, and the beam width could be accounted for.

Good luck... I doubt it. The most you can do is to get faster at off-setting. I am unaware of any programs designed for lasers that will do this. If you want strictly G code, you might be able to use a program such as Mastercam or Virtual Gibbs, and specify a .004 dia tool. You will have to do a lot of editing to make this work. Theoretically, you could do the automatic offsetting in the cam program, export it as a DXF, then import to corel.

The other "solution" is to use a narrower kerf width (using high density optics or a fiber laser) and live with the gap. On most jobs, the gap is not too unsightly, it's just that we engravers tend to be perfectionists!

Ted, the laser cutters we use are generally not designed for "part fabrication" although some of us have need make accurate parts. Many people can get away without ever compensating for kerf width and never calibrate their laser for accuracy, but some of us have projects that need more accuracy. The small laser systems don't use g-code; some of the larger flat-bed like Kern Lasers can accept g-code files.

I haven't found an easy way myself; like Mark suggested, you may have to just get more efficient.

Always keep master copies of the unmodified files - you will never be able to use kerf-offset files on different machines. Plus you may need to go back to the source file to make changes.

I haven't found an easy way myself; like Mark suggested you may have to just get more efficient.

With holes just copy the circle onto itself with the "+" key on the numpad, then reduce the diameter by kerf width (eg .005")

For outlines it is best if you have a closed path. Then offset out by 1/2* kerf. (Unfortunately in older versions of CorelDraw this creates a lot of nodes for offset shapes - I'm told X4 and X5 are better.) If you set up the offset parmaters so that the offset is a different color it is easier to keep track of which line to delete.

(I usually offset everything and then delete the original shapes - but as you know you need to remember that for holes, delete the OUTSIDE, on external features, delete the INSIDE.)

It is tedious to be sure.

If your files are too complex for manual offsets then I agree that creating an offset g-code file in another program and then converting the g-code back to to dxf SHOULD work in theory but pick your programs carefully. You may have to do a lot of experimentation to get it to work smoothly.

Doug, I don't think Ted meant that he was going to scale the drawing - I think when he said "bigger" he just mean with kerf offset applied. Seem Ted understands what is needed; just needs a way to do it efficiently.

There is a progam called DragonCNC which supposedly works with CorelDraw. I have NOT used it - but theoretically this could create the offset g-code in CorelDraw. But you still need to convert the file back to dxf to get it into a Corel file for the laser. If you currently have a CAM postprocessor that works with Solidworks that would be simpler. Then you still need the g-code to dxf converter to make it Corel-ready.

I converted from G-code and CNC's to laser cutting and was saddened that the laser drivers don't allow for kerf or Tool Radius Compensation. Instead, I manually offset each part depending on the thickness by 0.0035 to 0.005 in AutoCAD. It takes about two hours for 400 parts in one of my kits but then again, I have to put breaks in the lines too so that the parts won't fall out of the balsa sheets. So to take a model from assembled parts in a file to a properly formatted cutting file it takes about 8 hours.

AutoCAD 2000i does this offsetting pretty easily as you just select the offset tool and click on the part lines and then which side to offset on. It stays in that mode until you stop it so you don't have to reselect Offset every time. In that way offsetting 400 parts can be done in an hour or less. The major pain is zooming into each part to remove the original part. That takes a lot of mouse wheel work.

I'm thinking of a Corel macro that makes two copies of all lines, one with a negative offset and a second with a positive offset. All positives are on one layer, all negatives on another, both separate from the original... each layer has a different color for ease of view. A second macro is activated with a keypress, one of two keys, one deletes a positive offset layer object within a certain distance like 10 pixels (when you want to keep the negative), and vice versa for the other layer.

Setting up the macros may take a few hours, but once they're done, complete processing of a large file should only take an hour or so. Run the first macro to create the complete positive/negative layers, then hand edit the file using the second set of macros to selectively delete the offset you don't want (like keeping the negative offset for inside holes and deleting the hole's positive offset).

It would be one hell of a lot faster than manually editing each line. Oh, and Kay, we've had numerous discussions on how to keep tabs on cutout lines... do a search for some of them and you'll probably save yourself some time there, too. Adding tabs manually should be a last resort...

Change all your existing lines to construction (group select). Then use the offset command to set your offsets. When you do this it leaves your construction line and gives you a working line that is offset by the kerf amount. You can group select the lines for offset to the inner and for the offset to the outer.

This gives you the opertunity to just change the offset dimension for the parts and you get new kerfs for different beam widths

As far as using solidworks goes, You can start with your original part as one drawing configuration. Then add another configuration that has the kerf compensation built in. This would allow easy transition between CNC Mill and Laser exportation, and it keeps everything within one file reducing clutter. Think of drawing configurations as the closest thing you have in solidworks to using layers.
There is a check box in the offset dialog box that gives you the option of "select chain", "make the base construction." Once you have the new configuration, update the drawing then export it.